Hi I will like to ask whether SMD components can be used instead of the through-hole ones in your V3.0 parts list. Do advice on the power requirements for each component if so. Just figured maybe it'll have better power efficiency and super tiny flashdrive-sized PCB footprint. :wink:

I got the same open-circuit 4.98V at VCC of the USB, and 4.36V under iPhone 4/Galaxy S load. Voltage across the AA cells are 2.7V open-circuit, 1.65V under iPhone 4 load. Tried both Sanyo Eneloops and Energizer Alkaline.

Will test it on other devices with lower power demands later. Quite happy it worked though. :)

Edit: Forgot to add in the LT1302, I ordered the SOIC variant, LT1302CS8-5, free samples from Linear Tech.

Last edited by loongyh on Fri Oct 07, 2011 9:28 am, edited 2 times in total.

1. please do not call it mintyboost 3.0 - it will confuse folks since we do not offer a SMD version (yet) - SMDboost or something would be more appropriate.2. the forum photos are gigantic, you might want to resize them before posting.

adafruit wrote:1. please do not call it mintyboost 3.0 - it will confuse folks since we do not offer a SMD version (yet) - SMDboost or something would be more appropriate.

Oh sure, actually I called it that because the schematic is exactly the same as the mintyboost 3.0, just swapped the through-hole components with their equivalent SMDs.But I do understand the confusion it may bring. Not to worry though, I made only one currently and plan to test it out on a variety of devices first. I'll change its name to something else if I decide to manufacture it. :wink:

adafruit wrote:2. the forum photos are gigantic, you might want to resize them before posting.

Sorry about that! I thought this forum had automatic image resize feature. Just resized them already.

This is very cool! I have a few questions about it, since I am new to electronics. I would also like to make an SMD version because when I ordered samples of the lt1302 I got DIP and SMD types and I want to make use of them. I have tried to make a perf board MintyBoost with all thru hole components and it so far is an epic fail. I want next to try to custom design a pcb just like you did, for both the DIP and SMD chips. I have never done anything like this before, but I have all of the tools necessary. I usedhttp://www.expresspcb.com/'s software to design a hybrid board (SMD chip but thru hole components) and I just want someome to look it over and tell me if they think it will work. I know the admins wont help because they can't touch DIYers and thats fine, but if anyone would be willing to look I will post my designs. Thank you! Oh and what software is everyone using to make .brd files? I could only find the expresspcb and it doesnt save in that format.

I imported the schematic into eagle, replaced the components with their SMD equivalents, and routed the board manually in board mode. .brd is the board format for eagle. I don't really recommend newcomers to power electronics to design PCBs. Aside from thermal considerations, the high current from the power-carrying traces must be isolated from the traces which carry the high frequency signals from the switching regulator. Otherwise, EMI will be induced into the power lines, not very good for the load.

I discovered rather recently my board design is rather flawed. For one, it could have encompassed more copper on it, like ground plains, to aid in heat dissipation. Non-power and signalling traces can also be made with a smaller width, to aid in reducing EMI. The signalling traces must also be supplied with their own dedicated ground paths, the ground paths must not carry power current. Lastly, I designed the HF signals too close to the power traces. A killer for any device without noise filtering that connects to it. A good design will be something like this:

Basically, empty spaces are just blank copper and are left alone or connected to VCC or GND. All commercial PCBs manufactured, especially products involving HF signals, have similar designs. Some even has tiny holes drilled into them grid style, and vias connecting them to the other layers, which effectively turns the copper plains into a heatsink!

I've built the board over my free time last year as a second year electrical engineering student. I never even looked at the datasheet for the LT1302 and was totally clueless with what I was doing. However, I've learnt much over the year - my PCB designs of the previous were very flawed, with no thermal and EMI considerations.

Compare my board design to the reference design from the LT1302 datasheet:

Clearly, it shows just how clueless I was when I was routing the PCB. An obvious mistake is with the long and thick traces coming from the battery. Not only is there an added impedance, I believe the traces will also either emit EMI or act as an antenna to external EMI.

To quote a very important section on layout and thermal considerations from the datasheet:

LayoutThe high speed, high current switching associated with the LT1302 mandates careful attention to layout....High current functions are separated by the package from sensitive control functions. Feedback resistors R1 and R2 should be close to the feedback pin (pin4). Noise can easily be coupled into this pin if care is not taken. A small capacitor (100pF to 200pF) from FB to ground provides a high frequency bypass....The 0.1µF ceramic bypass capacitor C3 (use X7R, not Z5U) should be mounted as close as possible to the package....Grounding should be segregated as illustrated. C3’s ground trace should not carry switch current. Run a separate ground trace up under the package as shown. The battery and load return should go to the power side of the ground copper.

Thermal Considerations...For surface mount devices heat sinking is accomplished by using the heat spreading capabilities of the PC board and its copper traces. Experiments have shown that the heat spreading copper layer does not need to be electrically connected to the tab of the device. The PCB material can be very effective at transmitting heat between the pad area attached to pins 1 and 8 of the device, and a ground or power plane layer either inside or on the opposite side of the board. Although the actual thermal resistance of the PCB material is high, the length/area ratio of the thermal resistance between the layer is small. Copper board stiffeners and plated through holes can also be used to spread the heat generated by the device.

That was very helpful, I designed my pcb with consideration for the emi by including a rather large ground plane. I did not realize that this circuit would be difficult to redesign in all the other aspects. I'm not too worried about the circuit being the most efficient design possible as long as it functions. I can turn ALL of the excess space into a ground plane if it helps or ungrounded copper planes if there is no difference. Express pcb doesn't allow saving as an image so I could only post the .pcb files if someone was willing to look them over. I'll redesign the board with eagle for my own benefit right away and post them instead if I can get the hang of the software.

This is the best I can do until I learn how to use eagle. It seems far more complicated than Express pcb. Express was so easy. This is a screen shot of the pcb. Green is the bottom layer and red is the top layer. The odd shape is because of the tin I am fitting the project in. I am confident I have everything set up and connected to the right traces. I will work hard to get an eagle file up soon.

Update* I know I have the diode drawn backwards. I fixed that on my designs, but it's still backwards in the pictures.

Is the white space left for the battery holder? Actually, you can reduce the footprint of the PCB by more than half if you mount the PCB under the battery holder. Otherwise, the PCB looks very huge, and the traces are too long. The power traces for example can be thicker, or made into a power plane, refer to the reference design posted in my previous post.

I see you're using through-hole passive components too. Why not opt for their SMD variants? They have a much smaller footprint, which translates to smaller board and shorter traces. I'm thinking of using a double sided board, reserving the bottom layer just for the power and ground planes. :wink:

Yes the white space is where the batteries will go. I'm using a normal sized Altoids tin so that I can mount the usb port inside the case. From most angels you cant tell that there has been any alterations to the tin instead of the ladyada design having the port stick out of the tin. I thought it looked a little cooler. I supposed the L shape is not necessary. I will change the designs to shorten up the traces as much as possible and make a VCC plane along with my ground plane. I am using a double sided pcb because I couldn't design the traces well enough to make them all fit on one side. I didn't use SMD components for anything more than the chip because I already all of the components in through-hole style. If i order the components to make another Minty boost I will definitely use your list and go SMD for everything possible.

I printed my first double sided pcb today to practice. It isn't a functional circuit just a smiley face on one side and a frowny face on the other side. It worked out pretty well. Silly I know, but it's just practice.

It's great to know you're enjoying it! When doing pcbs, most importantly - have fun :) Double layer does simplify the routing process, however it adds a certain challenge during fabrication - the alignment has to be perfect.

I've completed the double-sided version, dubbed it SMDBoost rev. 2. It's less than half the size of the original, in fact, it's so small, the only way to manufacture it is through UV photoresist exposure. There's no way toner transfer can work on this.

I'm thinking of mounting the PCB on the side of a quad AA cell holder like this:

I ended up turning the empty space on both layers into ground planes. The power components go on top while the signalling components go below. Followed expresspcb's advice and selected the appropriate trace width based on current. Schematic remains the same, however the datasheet recommends placing a 24kohm resistor and 0.01uF capacitor on the Vc pin. Something to do with getting the best response. Ladyada's schematic consists of just a 0.1uF capacitor. Any thoughts on this?

I think I am going to send your v2 board off for my first manufactured PCBs (via OSHPark, formerly DorkbotPDX). Haven't had time to learn Eagle much yet, but looking to build a smaller Minty-derivative :-) Plus the surface mount inductor is way cheaper than the PTH.. wow!

You'll want to consider a power switch on the battery leads or a future rev of the PCB... there is some quiescent current draw with the LT1302 so storing your batteries in this will shorten their shelf life somewhat.